Fusion 360 Export Face to DXF

Simple script for Fusion 360 which will save a selected face as a DXF file. Useful for exporting 3d models to be used in programs like LightBurn for laser cutting.

Why

Fusion lets you export a sketch as a DXF, but there's a few issues here:

• DXF includes other sketch data, including lines which weren't extruded
• If multiple sketches were made on the same body, this export style won't work

Instead, what many people do is the following:

• Hide other components
• Select the face, and create a new sketch
• Use the "Project" tool (p key), and project the underlying geometry
• Finish the sketch
• Export this new sketch as a DXF

This workflow isn't terrible, but it is slow and a lot of button clicks. The below script just does all of these things automatically.

For example, take the following model, where I want to export the blue face:

The image on the left shows the default Save as DXF, the right shows the DXF output by this tool.

How to use

• Download the following script, save it as FusionLaser.py. Can save it anywhere, default location for scripts is: C:\Users\%USERNAME%\AppData\Roaming\Autodesk\Autodesk Fusion 360\API\Scripts.
• Go the the UTILITIES tab, ADD-INS, Scripts and Add-Ins
• Click the green + icon, and select the script

Then, to use it:

• Select the face you want to export
• Open this add-ins menu (or press Shift S)
• Select this script, and click Run
• A dialog box will prompt you to save the DXF. By default, it uses the parent component name

Script

import adsk.core, adsk.fusion, traceback
import os

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface
        des = app.activeDocument.design

        # get the selected face
        if ui.activeSelections.count != 1:
            ui.messageBox("Select a face")
            return

        selection = ui.activeSelections.item(0)

        selectedFace = selection.entity # should be a BRepFace object

        if not isinstance(selectedFace, adsk.fusion.BRepFace):
            ui.messageBox("Selected item is not a face")
            return

        component = selectedFace.body.parentComponent  # get the component the face belongs to

        # hide all other components
        for comp in des.allComponents:
            if comp != component:
                comp.isSuppressed = True

        # create a new sketch
        sketches = component.sketches
        sketch = sketches.add(selectedFace)

        # project face geometry
        for loop in selectedFace.loops:
            for edge in loop.edges:
                sketch.project(edge)

        # get default filename
        default_filename = component.name + ".dxf"

        # save file dialog
        file_dialog = ui.createFileDialog()
        file_dialog.title = "Save DXF File"
        file_dialog.filter = "DXF Files (*.dxf)"
        file_dialog.initialFilename = default_filename

        if file_dialog.showSave() == adsk.core.DialogResults.DialogOK:
            output_path = file_dialog.filename
        else:
            for comp in des.allComponents:
                comp.isSuppressed = False
            return

        # export the sketch as a DXF
        export_manager = des.exportManager
        dxf_options = export_manager.createDXFSketchExportOptions(output_path, sketch)
        dxf_options.filename = output_path
        export_manager.execute(dxf_options)

        #  unhide all components
        for comp in des.allComponents:
            comp.isSuppressed = False

        # delete sketch
        sketch.deleteMe()

        ui.messageBox('DXF exported successfully to:\n{}'.format(output_path))
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))